Plasticity
Use the Plasticity subnode to define the properties for modeling elastoplastic materials. This material model is available in the Solid Mechanics, Shell, Layered Shell, Membrane and Truss interfaces, and can be used together with Linear Elastic Material, Nonlinear Elastic Material, and Hyperelastic Material.
The Nonlinear Structural Material Module or the Geomechanics Module are required for this material model, and the available options depend on the products used. For details, see https://www.comsol.com/products/specifications/.
See also Elastoplastic Material Models in the Structural Mechanics Theory chapter.
Shell Properties
This section is only present when Plasticity is used as a subnode to:
•
Linear Elastic Material in the Layered Shell interface. See the documentation for the Plasticity node in the Layered Shell chapter.
•
Layered Linear Elastic Material in the Shell interface. See the documentation for the Plasticity node in the Shell and Plate chapter.
•
Layered Linear Elastic Material in the Membrane interface. See the documentation for the Plasticity node in the Membrane chapter.
Plasticity Model
Use this section to define the plastic properties of the material.
Plasticity Model
Select Small plastic strains or Large plastic strains to apply either an additive or multiplicative decomposition between elastic and plastic strains.
•
When using plasticity together with a hyperelastic material, only the option Large plastic strains is available.
•
When using plasticity in the Shell, Membrane and Truss interfaces, only the option Small plastic strains is available.
Yield Function F
The Yield function F defines the limit of the elastic regime F(σ, σys) ≤ 0.
Select a Yield function F criterion — von Mises stress, Tresca stress, Hill orthotropic plasticity, or User defined.
•
The default is von Mises stress with associate plastic potential.
•
Select Tresca stress to use a Tresca yield criterion. The plastic potential can be an Associated or nonassociated flow rule with the von Mises stress as plastic potential.
•
Select Hill orthotropic plasticity to use Hill’s criterion. For Hill orthotropic plasticity from the Specify list select either the Initial tensile and shear yield stresses σys0ij or Hill’s coefficients F, G, H, L, M, and N. The default for either selection uses values From material (if it exists) or User defined. The principal directions of orthotropy are inherited from the coordinate system selection in the Linear Elastic Material node.
•
For User defined enter a different value or expression. Write any expression in terms of the stress tensor variables or its invariants in the φ(σ) field.
-
For User defined also select the Plastic potential Q related to the flow rule — Associated, von Mises, or User defined (nonassociated). Enter a User defined value in the Q field as needed.
Initial Yield Stress
For all yield criteria, the default Initial yield stress σys0 uses values From material and represents the stress level where plastic deformation starts.
Isotropic Hardening Model
For all yield criteria, select the type of linear or nonlinear isotropic hardening model from the Isotropic hardening model list.
•
Select Perfectly plastic (ideal plasticity) if the material can undergo plastic deformation without any increase in yield stress.
•
For Linear the default Isotropic tangent modulus ETiso uses values From material (if it exists) or User defined. The yield level σys is modified as hardening occurs, and it is related to the equivalent plastic strain εpe as
with
For the linear isotropic hardening model, the yield stress increases proportionally to the equivalent plastic strain εpe. The Young’s modulus E is taken from the elastic material properties.
•
Select Ludwik from the list to model nonlinear isotropic hardening. The yield level σys is modified by the power-law
The Strength coefficient k and the Hardening exponent n use values From material (if it exists) or User defined.
•
Select Johnson-Cook from the list to model strain rate dependent hardening. The Strength coefficient k, Hardening exponent n, Reference strain rate , and Strain rate strength coefficient C use values From material (if it exists) or User defined.
Select a Thermal softening model — No thermal softening, Power law, or User defined.
-
For Power law, enter the Reference temperature Tref, the Melting temperature Tm, and the Temperature exponent, m.
-
For User defined, enter the Thermal Softening function f(Th), the Reference temperature Tref, and the Melting temperature Tm. The softening function f(Th) typically depends on the built-in variable for the normalized homologous temperature Th and have the properties f(0) = 0 and f(1) = 1. The variable is named using the scheme <physics>.<elasticTag>.<plasticTag>.Th, for example, solid.lemm1.plsty1.Th.
The yield stress and hardening function for the Johnson–Cook model is given by
In the case of power law softening, .
•
For Swift nonlinear isotropic hardening, the Reference strain ε0 and the Hardening exponent n use values From material (if it exists) or User defined. The yield level σys is modified by the power-law
Typically, the reference strain equals the onset of plasticity, ε0 =σys0/E.
•
Select Voce from the list to model nonlinear isotropic hardening. The yield level σys is modified by the exponential law
The Saturation flow stress σsat and the Saturation exponent β use values From material (if it exists) or User defined.
•
For Hockett-Sherby nonlinear isotropic hardening, the Steady-state flow stress σ∝, the Saturation coefficient m, and the Saturation exponent n use values From material (if it exists) or User defined. The yield level σys is increased by the exponential law
•
For Hardening function, the isotropic Hardening function σh(εpe) uses values From material or User defined. The yield level σys is modified as
-
This definition implies that the hardening function σh(εpe) in the Material node must be zero at zero plastic strain. In other words, σys = σys0 when εpe = 0. With this option it is possible to enter any nonlinear isotropic hardening curve. The hardening function can depend on more variables than the equivalent plastic strain, for example the temperature. Select User defined to enter any function of the equivalent plastic strain εpe. The variable is named using the scheme <physics>.epe, for example, solid.epe.
Kinematic Hardening Model
For all yield function criteria, select the type of kinematic hardening model (not available for hyperelastic materials) from the Kinematic hardening model list.
•
Select No kinematic hardening (when either ideal plasticity or an isotropic hardening model is selected as isotropic hardening model) if it is a material that can undergo plastic deformation without a shift in the yield surface.
•
If Linear is selected as the Kinematic hardening model, the default Kinematic tangent modulus Ek uses values From material. This parameter is used to calculate the back stress σb as plasticity occurs:
with
This is Prager’s linear kinematic hardening model, so the back stress σb is collinear to the plastic strain tensor εp.
•
If Armstrong-Frederick is selected from the list, the default Kinematic hardening modulus Ck and Kinematic hardening parameter γk use values From material. These parameters are used to calculate the back stress σb from the rate equation
This is Armstrong–Frederik nonlinear kinematic hardening model. Replacing the variable for the back strain instead of the back stress
gives the rate for the back strain
•
When Chaboche is selected from the Kinematic hardening model list, the default Kinematic hardening modulus C0 uses values From material. Add branches as needed to solve N rate equations for the back stresses:
or equivalently, solve N rate equations for the back strain such as
The total back stress σb is then computed from the sum of the branches
For each Branch row, enter Ci (the hardening modulus of the branch i) in the Hardening modulus (Pa) column and γi (the hardening parameter of the branch i) in the Hardening parameter (1) column.
Use the Add button () and the Delete button () to add or delete a row in the table. Use the Load from file button () and the Save to file button () to load and store data for the branches in a text file with three space-separated columns (from left to right): the branch number, the hardening modulus for that branch, and the hardening parameter for that branch.
To compute the energy dissipation caused by plasticity, enable the Calculate dissipated energy check box in the Energy Dissipation section of the parent material node.
•
Sheet Metal Forming: Application Library path Nonlinear_Structural_Materials_Module/Plasticity/sheet_metal_forming
•
For an example of Large plastic strains, see Necking of an Elastoplastic Metal Bar: Application Library path Nonlinear_Structural_Materials_Module/Plasticity/bar_necking.
•
For an example of strain rate dependent plasticity, see Tensile Test with Strain Rate Dependent Plasticity: Application Library path Nonlinear_Structural_Materials_Module/Plasticity/strain_rate_dependent_plasticity
Location in User Interface
Context Menus
Solid Mechanics>Linear Elastic Material>Plasticity
Solid Mechanics>Nonlinear Elastic Material>Plasticity
Solid Mechanics>Hyperelastic Material>Plasticity
Shell>Layered Linear Elastic Material>Plasticity
Layered Shell>Linear Elastic Material>Plasticity
Layered Shell>Hyperelastic Material>Plasticity
Membrane>Linear Elastic Material>Plasticity
Membrane>Layered Linear Elastic Material>Plasticity
Membrane>Nonlinear Elastic Material>Plasticity
Truss>Linear Elastic Material>Plasticity
Ribbon
Physics tab with Linear Elastic Material, Layered Linear Elastic Material, Nonlinear Elastic Material, or Hyperlastic Material node selected in the model tree:
Attributes>Plasticity